Modeling Challenge – 3D Wireframe Sketch

*This is one part of a series of modeling challenges you can use to test your SOLIDWORKS skills. First, read the challenge and try to figure out a solution on your own. Then, compare your solution with my good, better, and best recommendations. As always, feel free to share even more tips and tricks in the comments below.

Before solid modeling, CAD users were forced to generate wireframe representations of solids. Solids trump wireframes almost always, but what should you do when you need a wireframe representation of a shape? One common use case for wireframes are the sketches that drive our Structural Member features for Weldments. For this challenge, let’s determine the easiest way to create a 3D wireframe sketch for the frame of a tunnel-like canopy as shown below.

modeling challenge - Weldment

Multiple 2D Sketches

Most people look at the shape above and immediately think, “3D Sketch”. Though 3D sketches are capable of creating complex shapes, so can multiple 2D sketches. Best of all, 2D sketches allow us to stick to an environment we’re most familiar and comfortable with. As far as downstream weldment features go, Structural Members do not care whether you use multiple 2D sketches or a single 3D sketch as long as each entity is where it needs to be.


  1. Create a profile sketch (on the Front plane)
  2. Create a sketch that represents the path segments of the tunnel (on the Top plane)
  3. Create a plane coincident and normal to the endpoint of one of the path segments
    A fast way to do this is to customize your Context-Sensitive Toolbar to include the Plane command. Then you can Ctrl+Select the line segment and the endpoint, then simply click the Plane icon from the Context-Sensitive Toolbar, and click OK to accept the new Plane.
  4. Ctrl+Select the profile sketch and the new plane
  5. Select ‘Insert’ > ‘Derived Sketch’
    Derived Sketches are an easy way to duplicate a master sketch multiple times on any face/plane/position throughout the model. Any edits to the master sketch will immediately update all of the derived sketches.
  6. Edit the new derived sketch and fully define its position
    Usually this step can be completed with a couple of coincident or horizontal/vertical sketch relations, but don’t forget about the Modify Sketch tool in case you want to flip or rotate the sketch’s position.
  7. Create another plane parallel to the Top plane and Coincident with one of the endpoints of the arc entities
  8. Repeat steps 4-6 to create a Derived Sketch for the path segments
  9. Create a plane through three points of the intermediate cross section of the tunnel
  10. Create a sketch on the new plane to connect the dots with two vertical lines and one arc across the top

There are only two things wrong with this workflow. First, it requires tedious work generating all of the individual planes and sketches. Second, just sketching “one arc across the top” won’t provide a geometrically accurate representation of the true cross sectional profile at that point. Instead, you’d have to create some additional geometry and use either the Project Curve or Intersection Curve commands.

3D Sketch

If you’re one of the few that are more comfortable sketching this shape in a single 3D sketch rather than multiple 2D sketches, you would know the workflow wouldn’t be that different from the one above. The only big differences would include:

Sacrificial Solid Body Driven 3D Sketch

The intriguing part about this modeling challenge is that if I originally asked you to create this shape as a solid model, almost everyone would answer it the exact same way – sweep the profile along a path. So if that solution is so straightforward and fast, why don’t we try to use it?


  1. Sweep the solid geometry
  2. Create a 3D Sketch
  3. Select one of the model’s edges
  4. Click Ctrl+A to select all of the model’s edges
  5. Use the Convert Entities tool to convert all of the model’s edges into sketch entities
  6. Delete any unnecessary sketch entities and exit the sketch
  7. Use the Delete Body command to remove (i.e. sacrifice) the solid body
    The easiest way to activate this tool is to expand the ‘Solid Bodies’ folder, highlight the body, and click the Delete key on your keyboard

This solution is fast, familiar, and very easy. The best part is there are no confusing 3D sketch relations to maintain and your FeatureManager tree doesn’t get littered with unnecessary planes. When it’s time to make a change to the shape, just roll the rollback bar up above the Delete Body feature and edit away. Once you roll the rollback bar back down, you’ll notice the 3D sketch is automatically updated!

Sacrificial bodies are beneficial in many ways. Any time you find yourself generating more planes than you care to create, ask yourself, “Would it be easier to sketch on the faces of a single solid body rather than a ton of planes?”  For example, check out the garage design below.  By creating a sacrificial solid body first, not only do I have a great visual prototype of the design, but I also have all of the faces to create my Structural Member sketches on with minimal upfront work.


Jordan Tadic

Jordan Tadic

Territory Technical Manager - NA East at SOLIDWORKS
Jordan has been serving the SOLIDWORKS community for over 10 years. He’s a mechanical engineer by day and a wannabe artist by night, so he’s at his best when he’s forced to use both sides of his brain to solve complex modeling challenges. If you have one for him, don’t hesitate to share it. His specialties are surface modeling, industrial design, cloud solutions, and technical communications.
Jordan Tadic
Jordan Tadic